Thin metal circular disk-FEM results reliability 3

[Alekos91]

Hello,

I use ANSYS Workbench for mechanical stress analysis of a thin metal circular disk (Diameter=700mm, Thickness=10mm) with some air gaps and a hole in the center (please see pics) subjected to bending. The results that I get for the equivalent von-Misses stress show me that in a very small region near the air gaps' corners the stresses are much larger than the yield strength( 235MPa) I tried to change the mesh (size and element type), and the boundary conditions but the results do not change significantly. The disk has been constructed and works properly with no sign of failure.

So the problem is: Is my model reliable? Is it possible the constructed disk to encounter such big stresses in such small regions without breaking? Can I trust the results of Ansys? Or there is something wrong I have done when I constructed the mesh..?

Sorry for the bad structure of the post, I am new to the forum..

Thank you in advance!

 

[corus]

At such a stress concentration feature the stresses are classed as a peak stress that leads to failure through fatigue damage, ie. cracking. The acceptability of such stresses doesn't depend on whether it exceeds yield or not but on the number of cycles and the stress range. Refer to design codes to assess the stresses.

 

[Alekos91]

Thank you corus for your answer. You made it clear in my mind.

Do you have any idea of which code is appropriate for such an application?

P.S. The disk is actually the rotor of an AFPM electric generator of a smal wind turbine.

 

[rb1957]

There could well be a stress concentration problem, but you need to run your fatigue loads (as opposed to your extreme design loads) or it may an artifice of the linear FEA ?

another day in paradise, or is paradise one day closer ?

 

[Alekos91]

Thank you for your post but I have some questions:

1)What is the meaning of ''fatigue'' analysis as long as I have a static load, not a dynamic one?
2) What do you mean exactly by ''artifice of the linear FEA''

 

[aerostress82]

I'll just add here but rb1957 is more knowledgeable with stress generally, so I'd take his answer into consideration as well.
Comment for 1 only):
Your "service/fatigue" and your "ultimate (abuse)" loads are generally different in structures. For instance, you might have a 100lbs of fatigue loading for a structure - whereas your ultimate/abuse loading may be 250lbs.



If you already have already applied your fatigue loading in your analysis, then you might have a "surface finish factor" that you need to take into account. I'm not a fatigue expert but surface finish factors may affect the fatigue analysis results significantly. So, your actual physical model may not be failing due to this effect.

You may also want to check your surface finish factor while performing a "fatigue analysis" with your service/fatigue loading. (ie. 100 lbs I mentioned above - depending on your own structure's requirements)

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[corus]

For fatigue assessment the design code (in the UK) is BS7608. There are similar codes in ASME. Look at this site for further details,

http://www.twi-global.com/technical...ign-rules-for-welded-structures-january-2000/

The loading on the structure doesn't necessarily have to be a dynamic load, but a repeated 'static' load that causes failure.

In general these codes use the calculated linear stress rather than stresses calculated using non-linear plastic analysis.

Surface finish does have an effect on fatigue damage as well as environment, and in other cases the proximity to welds.

 

[gravityandinertia]

I believe it's an "artifice of linear FEA" as rb1957 implied. What he means is that in a linear static analysis the assumption is that the material always has a stiffness proportional to Young's Modulus (Modulus of Elasticity), but when the yield is exceeded that is no longer true. What happens in those case is the slope of the stress-strain curve is reduced dependent on the strain. Compared to Linear static analysis, a non-linear analysis that takes this into consideration would predict larger strains around those corners, but lower stresses (still beyond yield). It would also tell you the permanent strain in those corners after the initial loading/unloading.

What would happen is the stress would redistribute over a larger area in those corners as they passed the yield strength.

 

[rb1957]

exactly, you can't chase stress from a linear FEA up the peak of a stress concentration. The result is meaningless as plasticity occurs. Once you see this happening you can ...
1) rerun with material non-linearity (elastic/plastic material stress/strain), or
2) if this is a fatigue analysis, maybe use the stress peak to infer a stress concentration factor, or
3) ignore it ... it is a result of the running a highly non-linear problem (a stress concentration) with a linear FEA.

You might investigate how much material is expected to yield ? Plot the stress results, then cut-off at yield stress, so you have truncated the stresses at yield. Now the area in the stress results curve above yield needs to get reflected in this truncated analysis. You can increase the stress near the edge of the truncated stress, so that you add the same area as was removed with the truncation ... clear as mud ?

another day in paradise, or is paradise one day closer ?

 

[Alekos91]

Ok. I think I understood some things deeper.

1)I runed a non-linear analysis and I got a contour with the plastic strain one with the stresses. But how can I now decide if the plastic area is big enough to cause the failure of the disc? Is there an upper allowable limit for the plastic strain for example?

2)I have a static constant load, neither a dynamic nor a repeated one. So I think there is no meaning of fatigue analysis.

3) That's what I will probably do at the end.

Thnx for your answers!

 

[gravityandinertia]

For item 1, you would look at the stress value. Does it get close or exceed the ultimate strength of the material? That would determine your failure.

Of course is failure is related to some sort of geometric change, then you would also have to decide if the permanent deformation caused by the plastic strain produces operational issues for this particular item.